Material SFM Chart
Material Cutting Speed Reference Chart
Find a starting SFM or Vc by material, compare machinability, and then move into RPM and process-specific calculators. This page is the chart layer, not the final programmed feed-and-speed answer.
Direct answer: choose a material SFM or Vc range first, convert that speed to RPM by diameter, then validate feed, chip load, MRR, and process-specific limits.
Use this chart to choose material cutting speed before conversion. Use it before the SFM to RPM calculator, not as a substitute for milling, turning, drilling, or feeds-and-speeds calculators.
Use this chart to choose a starting material SFM/Vc range, then move into RPM, chip-load, MRR, and power validation.
Reference role: choose material cutting speed before spindle-speed and feed calculations. Convert SFM or Vc to RPM, then branch into the process calculator that matches the operation.
SFM, RPM, and MRR Decision Path
Follow this path from material speed lookup to spindle-speed conversion, formula review, live MRR calculation, and optimization guidance.
What This Page Covers Best
Use it as a material SFM chart when you want a realistic starting cutting speed before plugging in tool diameter or process-specific feed logic.
What It Does Not Replace
This page does not replace chip load, IPR, peck cycle, or boring-overhang decisions. Those still belong in the dedicated calculators after you pick a material speed.
After Speed Selection
After choosing an SFM range, move to the RPM calculator, then into the correct process page for turning, drilling, or general feeds and speeds.
Formula Chain Before You Program the Cut
Formula chain: SFM or Vc -> RPM -> chip load -> feed rate -> MRR. Use this table to choose the material speed, then move through the calculators in order so the final feed and removal-rate numbers still match the actual cutter, flutes, engagement, and machine limits.
Worked example: 4140 steel at 500 SFM with a 0.5 inch end mill is about 3,820 RPM before feed and power checks. Feed check: at 4 flutes and 0.003 inch chip load, table feed is about 45.8 IPM. If the machine cannot hold that speed under load, cap RPM first and recalculate the real surface speed before approving chip load or MRR.
Worked example handoff: after selecting 4140 steel at 500 SFM, convert diameter to RPM, calculate chip-load feed, then send feed and engagement into MRR before checking power.
How to Read This Reference
Step 1: Find Your Material
Locate the material group and specific alloy in the Master Table. Check the machinability rating — higher % = easier to machine.
Step 2: Choose Your Coating
Cross-reference the Coating Guide to select the right insert coating. Apply the speed multiplier to the base SFM value.
Step 3: Calculate RPM
Use RPM = (SFM × 3.82) / Diameter (inches), or go straight to the RPM & cutting speed calculator.
Step 4: Route Into the Right Process
Once RPM is set, move into the dedicated calculator for your operation: turning, drilling, or general feeds & speeds.
Note: These are starting parameters for uncoated carbide tools. Coated carbide (TiAlN, AlTiN) can typically run 20-50% faster. High Speed Steel (HSS) should run at 40-50% of these speeds. Always verify on your specific machine with a test cut, then carry the result into the correct process calculator for feed and DOC decisions.
Master Cutting Speed Reference (with Machinability)
| Material Group | Common Grades | Machinability | Milling (SFM) | Turning (SFM) | Vc (m/min) | Kc (N/mm²) |
|---|---|---|---|---|---|---|
| Aluminum Alloys | 6061, 7075, 2024 | 300% | 600 - 1500+ | 800 - 2000+ | 180 - 600 | 700 |
| Cast Aluminum | A356, 380 | 200% | 400 - 1000 | 500 - 1200 | 120 - 360 | 650 |
| Free-Machining Steel | 12L14, 1215 | 100% | 400 - 700 | 500 - 800 | 120 - 240 | 1500 |
| Low Carbon Steel | 1018, A36 | 78% | 350 - 600 | 400 - 700 | 100 - 210 | 1800 |
| Medium Carbon Steel | 1045, 4140 (Ann.) | 60% | 300 - 500 | 350 - 600 | 90 - 180 | 2100 |
| Alloy Steel (Hard) | 4140, 4340 (30-40 HRc) | 40% | 150 - 300 | 200 - 400 | 45 - 120 | 2800 |
| Tool Steel | D2, H13, A2 (45-55 HRc) | 25% | 80 - 200 | 100 - 250 | 25 - 75 | 3200 |
| 303 Stainless (Free) | 303 | 65% | 250 - 500 | 300 - 550 | 75 - 165 | 2200 |
| 300 Series Stainless | 304, 316L | 45% | 150 - 350 | 200 - 450 | 45 - 135 | 2500 |
| 17-4PH (H900) | 17-4PH, 15-5PH | 35% | 120 - 280 | 150 - 350 | 35 - 105 | 3000 |
| Titanium Alloys | Ti-6Al-4V (Gr.5) | 22% | 120 - 250 | 150 - 300 | 35 - 90 | 1400 |
| Inconel / Nickel | 718, 625, Hastelloy | 12% | 40 - 100 | 60 - 150 | 12 - 45 | 3200 |
| Free-Cutting Brass | C360, C385 | 300% | 500 - 1500 | 600 - 2000 | 150 - 600 | 800 |
| Pure Copper | C110 (ETP) | 20% | 200 - 500 | 250 - 600 | 60 - 180 | 900 |
| Gray Cast Iron | Class 30, Class 40 | 70% | 250 - 400 | 300 - 500 | 75 - 150 | 1100 |
| Ductile Iron | 60-40-18, 80-55-06 | 55% | 200 - 350 | 250 - 400 | 60 - 120 | 1600 |
| Delrin / Acetal | POM, Acetal | 500% | 600 - 1200+ | 800 - 1500+ | 180 - 450 | 350 |
| Nylon | PA66, PA6 | 400% | 500 - 1000 | 600 - 1200 | 150 - 360 | 300 |
| PEEK | PEEK 450G | 200% | 300 - 800 | 400 - 900 | 90 - 270 | 400 |
Machinability: Relative to AISI B1112 free-machining steel (100%). Kc: Specific cutting force in N/mm² — used for power calculations. Values are for uncoated carbide, roughing conditions.
Tool Coating Selection Guide
| Coating | Speed Multiplier | Max Temp | Best Materials | Avoid With |
|---|---|---|---|---|
| Uncoated Carbide | 1.0× | 650°C | Aluminum, copper, plastics | Hardened steel, superalloys |
| TiN (Gold) | 1.15-1.25× | 600°C | Carbon steel, low-alloy steel | Aluminum (BUE), high-temp alloys |
| TiCN (Blue-Grey) | 1.20-1.30× | 400°C | Stainless, medium-carbon steel | Cast iron (dry), aluminum |
| TiAlN | 1.30-1.50× | 800°C | Steel, stainless, dry machining, high-temp alloys | Aluminum (BUE risk) |
| AlCrN | 1.35-1.55× | 1100°C | Titanium, Inconel, hardened steel (>50 HRc) | Low-speed ops, aluminum |
| ZrN (Gold) | 1.15-1.30× | 600°C | Aluminum (prevents BUE), brass, copper | Steel, stainless |
| DLC (Diamond-Like) | 1.50-2.00× | 400°C | High-Si aluminum, composites, graphite | Ferrous metals (diffusion) |
| PCD | 2.00-3.50× | 700°C | Aluminum (production), composites, ceramics | All ferrous metals |
TiAlN is the most versatile coating for general-purpose steel/stainless machining. For detailed guidance, see our Tool Coating Selection Guide.
Thermal Conductivity & Chip Characteristics
Thermal conductivity determines how heat is distributed during cutting. Low-conductivity materials concentrate heat at the cutting edge, causing rapid tool wear. This is why titanium and Inconel require specialized approaches.
| Material | Thermal K (W/m·K) | Heat Rating | Chip Type | Coolant Recommendation |
|---|---|---|---|---|
| Copper C110 | 390 | Excellent | Continuous, stringy | EP fluid for chip control |
| Aluminum 6061 | 167 | Good | Continuous, curled | Flood or MQL (BUE prevention) |
| Brass C360 | 115 | Good | Short, broken (ideal) | Often dry, air blast |
| Cast Iron Cl.30 | 46 | Medium | Discontinuous (dust/chips) | Usually dry + vacuum |
| 1045 Steel | 50 | Medium | Continuous, snarled | Flood water-soluble |
| 304 Stainless | 16 | Poor | Continuous, work-hardened | Flood required, never dry |
| Ti-6Al-4V | 6.7 | Very Poor | Segmented, sharp edges | HP coolant (70+ bar) mandatory |
| Inconel 718 | 11.4 | Very Poor | Segmented, spring-back | HP coolant + ceramic/CBN tools |
Frequently Asked Questions
What is machinability rating and how is it used?
Machinability rating compares a material's ease of machining to AISI B1112 free-machining steel (rated 100%). Higher ratings mean easier machining, longer tool life, and higher allowable speeds. Aluminum 6061 rates ~300% (very easy), 304 stainless rates ~45% (difficult), and Inconel 718 rates ~12% (very difficult). Use the rating to proportionally scale speeds and predict relative tool life.
Which tool coating should I use for my material?
TiN (gold) for general steel. TiAlN for high-temp alloys and dry machining — the most versatile coating for steel/stainless. AlCrN for titanium and hardened steel (>50 HRc). ZrN or uncoated for aluminum (prevents built-up edge). DLC or PCD for composites and high-silicon aluminum. The right coating can increase tool life by 200-500% and allow 30-50% higher speeds.
Why does thermal conductivity matter in CNC machining?
Materials with low thermal conductivity (titanium: 6.7, Inconel: 11.4 W/m·K) concentrate heat at the cutting edge, causing rapid crater wear and tool failure. Materials with high conductivity (aluminum: 167, copper: 390 W/m·K) dissipate heat through the workpiece and chips, allowing much higher speeds. This is why titanium requires high-pressure coolant and lower speeds despite being lighter than steel.
What is Kc (specific cutting force) and why is it listed?
Kc is the force (in N/mm²) required to remove a 1mm² chip cross-section. It determines power requirements: Power (kW) = Kc × MRR / (60,000 × η). High Kc materials (Inconel: 3200, hardened steel: 2800) need more spindle power per unit of MRR. Low Kc materials (aluminum: 700, plastic: 350) cut more easily with less power.
How do I convert between SFM and Vc (m/min)?
SFM × 0.3048 = Vc (m/min). Or Vc × 3.281 = SFM. Example: 800 SFM for aluminum = 800 × 0.3048 = 244 m/min. Then RPM = (Vc × 1000) / (π × D_mm) or RPM = (SFM × 3.82) / D_inches. Our RPM Calculator handles all conversions.
Should I machine stainless steel dry or with coolant?
Always use coolant for austenitic stainless (304, 316). These grades have extremely low thermal conductivity (16 W/m·K) and work-harden rapidly. Dry machining causes the cutting zone to overheat, forming a hardened layer that destroys the next cutting edge. Use flood coolant, maintain constant feed (never let the tool rub), and ensure chip evacuation. Exception: 303 free-machining stainless tolerates MQL in some operations.
RPM & Cutting Speed
Convert the material SFM chart into spindle RPM for your actual tool diameter before you touch feed or chip load.
CNC Turning Calculator
Dedicated lathe calculator with insert selection, surface finish prediction, and 22+ materials.
Drilling Calculator
Turn the material-speed starting point into drilling RPM, feed, peck cycle, and depth guidance.
Chip Load Calculator
Check feed per tooth after RPM is known, before increasing table feed or MRR targets.
Material Removal Rate
Convert depth, width, and feed into removal-rate and spindle-load pressure.
Cutting Formula Guide
Audit the SFM, RPM, feed-rate, chip-load, and MRR formulas before release.